The Freeform tool in SolidWorks is used to modify an existing planer or non-planer surface/face of a body. The Freeform tool allows designers to morph a simple surface into a more complex surface in less time than using the standard Surfacing tools and also keeps the feature tree clean. This tool provides you with direct interactive control over the deformations that you want to create. Use the Freeform tool to add points on the surface which will act as a pick point and then move those points around in any direction to modify the surface
The freeform tool is used to make Class A surfaces in different kinds of fields such as automotive design, aerospace design, etc. Most commonly, it is used in consumer product design where highly aesthetic shapes are required such as ergonomic handle grips, car bodies, or organically shaped home appliances.
Freeform provides more direct control when compared to the Deform feature hence it is used more frequently. You can modify mostly any type of surface with any number of sides with the help of this tool but there are some exceptions to it. Like you can’t modify closed revolved faces such as a spherical face or the revolved face of a cylinder etc. with this tool. Also, you can only modify one face at a time using this tool.
In order to create a freeform feature follow the steps given below:
1. Open a part file that has the surface/face to which you want to add the freeform. It might be helpful to have a reference sketch or a sketch picture to base the freeform on.
2. Click the Freeform tool present in the Surfaces as well as the Features toolbar or go to Insert > Features > Freeform.
3. In Face to Deform, select the face that you want to modify.
Select Direction 1 Symmetry if you want your face to be symmetric. A plane will appear along which the symmetry will be propagated. The tool automatically adds control curves/points in the direction across the line of symmetry of the face. Use this option to design one half of the model and let Freeform symmetrically apply the design to the other half.
Note: Direction Symmetry is only available if the mesh of the face is symmetrical in one direction. Use this option to design one quadrant of the model and let Freeform symmetrically apply the design to the whole model.
Direction 2 Symmetry is only available if the face is symmetrical in two directions as defined by the mesh. Lets you add symmetric control curves in the second direction.
4. Next let us set the Continuity callouts. There will be one continuity callout on each side of the face. The continuity callouts help control the relation of the modified face to the original face. The Continuity callout is applied to the entire edge it belongs to.
- Contact: The edge will maintain its contact along the original boundary. You cannot move the edge if this option is selected. Tangency or curvature will not be maintained.
- Tangent: This option forces the edge to maintain the tangency with the original face. For example, if the face originally made an angle of 30° where it meets the boundary, the angle will be maintained after you modify the face.
- Curvature: This option forces the edge to maintain the curvature of the original face. For example, if the face originally had a normal radius of curvature of 10 meters with a plane along the boundary, that same radius is maintained after you modify the face.
- Moveable: This option allows you to move the edge itself. Neither the original boundary nor the original tangency is maintained. You can drag and modify the boundary using control points just like you can modify the face. Select a boundary handle or point and drag it to move it.
- Moveable/Tangent: This option also allows you to move the edge but you can do so while maintaining the tangency with the original face. You can drag and modify it using control points like you can modify the face. Select a boundary handle or point and drag it to move it.
5. Adjust the display of the face by adding transparency, zebra stripes, mesh preview, or curvature combs. While these options do not affect anything in the model itself but will help you place control curves/points more accurately and will also help you to notice the small changes more easily.
6. Now, let us add some control curves. These control curves will be used to modify the face. Click on the Add Curves button to activate it and then hover over the selected face. A preview curve will be shown in green. Use the Flip direction button to change the direction of the preview curve. Use left-click to place the curve. Place as many curves as required but try not to add too many curves. After you have finished adding all the curves click again on the Add Curves button to deactivate it.
7. Now select the control type:
- Through Points: Uses control points on control curves. Drag the control points to modify the face.
- Control Polygon: Uses control polygons on control curves. Drag the control polygon vertices to modify the face.
8. Now click on the curve in the graphics area that you placed on the face to select it.
In the case of the Through Points option, two handles will appear at the endpoints of the curve. You can now drag that handle to modify the face. Additional points may also be available if your curve is being intersected by any other curve from the other direction. You can also move these points to change the shape of the face.
If you have selected the Control Polygon option then you will find that the control curve will now work as a Style Spline. You can then edit the curve as if it were a style spline by moving the control vertices.
9. You can always add additional control points to the control curves. Under the Control Points menu, there is an Add Points button available which allows you to add as many control points as you want to allow finer control on the curve. Note that the Control points can only be placed on the Control Curves that are already present on the face. You can’t add control points at random places. Use the grid lines to help match the points. Additionally, you can use the Snap to geometry option to allow the control point to automatically snap to existing geometry such as points on a reference curve. The triad’s center changes its color to let you know that the point has been snapped to the geometry.
10. After you are done adjusting the face, click Ok to let the Freeform tool apply its magic. If you don’t like the end result or want to change the shape further, you can always right-click on the Freeform feature in the Feature Manager Design tree and select Edit Feature to change the parameters.
And that’s it. We hope that this article helped you learn how to use the Freeform tool in SolidWorks. If you have any questions or suggestions, feel free to leave a comment down below.